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Hey all...I am having a problem with a round feature in a part I am designing. In short, the feature keeps failing and I can't figure out why. I've attached a copy of my part. Refer to 'Round 7' in the model tree. If you can figure out how to make this work, please let me know. Thanks.
Solved! Go to Solution.
Here is your part, I believe finished.
I assumed you're cutting the ribbing with a ball mill so I modeled accordingly
As I mentioned earlier, I reordered some features, eliminated some double definitions and only added one additional feature. - round 8
The sketch that failed on me was missing the sketch plane definition. as soon as I selected the correct plane, all else worked.
enjoy
Mark,
I think you cannot create Round as Solid feature. Create it as Surface and close the space between round and model geometry.
MH
first, I switched trajectory ribs
I then moved failed feature - round 7 - under rib 2
created a new fillet (opposite of round 7)
went into feature round 3 and removed the duplicate definition of round 7 and new fillet
now it fails at sketch 2 and I don't have anymore time to play with it
That won't work if there's draft.
Makes it easier then! Unfortunately, everything I've had to do for the last 4+ years has draft everywhere, I can't open any of these files so I can't tell if there's any or not. Which is why I said "if". Ah well, but that's what makes designing IM plastic parts so "fun"!
Add a small extrusion to create a continuous surface at the top, first.
Then the round will solve itself.
Change the transition stop case...
Click on the red highlight at the top of the preview and the options will be available.
I wasn't sure if you were trying to get a controlled radius or a full round to the center boss.
Either way, the software is a bit finicky on the second instance.
Creating both rounds in a single feature makes this work.
The video will show how I was struggling to get either possible results.
Thanks Antonius...I tried this approach too and it worked great. It's a little cumbersome but seems to work just fine.
Here is your part, I believe finished.
I assumed you're cutting the ribbing with a ball mill so I modeled accordingly
As I mentioned earlier, I reordered some features, eliminated some double definitions and only added one additional feature. - round 8
The sketch that failed on me was missing the sketch plane definition. as soon as I selected the correct plane, all else worked.
enjoy
Thanks Ron. I hadn't tried re-ordering features in the model tree but this definitely did the trick.